Hello, The following is my reply to the TTM Technologies Technical Query: Date 9-March-2017 Customer No. 40-00624-00LF Site Tooling P/N 170892 I have generated new Solder Mask and Plugs gerber plots. - The new Solder Mask plots should fix the "tenting" caused by mask clearance problems as noted in Issues #5 and #6. - The new Plug plots have added plugs on the top side of the card under the 10 Ethernet Transformers. I think that these additional plugs may be helpful during assembly. - These 4 new Hub Module gerber plots are on the web at: http://www.pa.msu.edu/hep/atlas/l1calo/hub/hardware/manufacturing/Production/Bare_Board/ please see artwork files: 19, 20, 23, 24 Except for Issue #8, I believe that most of the issues are now understood. Debron, please let me know if there are any changes that you would like to facilitate the card assembly, e.g. additional plugs under the BGAs as was asked about at the end of Issue #6. Thank you all for your help with this card, Dan Issue #1 Please see an attached Gerber Data For Your Approval. Answer: Can we discuss the other points first and then decide which Gerber Data should receive final approval. Issue #2 We will Provide ENIG (Immersion Gold) Per IPC-4552, Which is 118 Micro-Inches of Minimum Nickel Followed by 2 Micro-Inches of Minimum Gold.Please Confirm. Answer: Debron please comment, is this the best type of surface finish for you to work with ? Whatever is best for you is fine with me. Issue #3 We will Build this Part Per IPC 6012 Class 2 Per Quotation.Please Confirm. Answer: Correct, IPC class 2 is what I was expecting. Debron, is this what you are expecting ? Issue #4 The milling on bottom side is cutting 2 holes at R958 and mounting hole on rail as shown in the image. Please advise if this is acceptable or not. Image Answer: Milling part of the via near the lower right hand corner next to R958 is acceptable. It is my mistake to have placed this via where it is but it is OK if this via is cut. Can you stop the milling, along both the Top and Bottom edges, 20 mm short of the left-hand edge of the card ? This will leave the at risk holes adjacent to the left-hand edge fully intact and will still let us insert the card into the card guides. Issue #5 One 2.7 mm pth hole is tenting by solder mask on top side as shown in image. We have added a mask clearance the same as on bottom side to open it up. Please advise if this is acceptable. Image Answer: I have made new Solder Mask plots that now include mask relief for this pth hole. Issue #6 As per drawing note there is no solder mask "tenting" of any of the vias or component pin holes. However in the data on top side the vias under BGA Meg_S1, Meg_s2, U1, U25, Trn_MP1, Rec_MP2, and all TRANS# are tented by solder mask. On bottom side the vias under U504, U507 and DCDC9 are tented by mask too. For these via holes we have added a mask relief of drill +6 mil to the tented side. As per via plug layers, the U504, U507 and DCDC9 are to be plugged, please advise if via plug is required for the BGA devices or not. Answer: In the new Solder Mask plots I have corrected the problem of the missing mask clearance on the Top side for the vias under: BGA Meg_S1, Meg_s2, U1, U25, Trn_MP1, Rec_MP2, and all 10 TRANSs. These vias are no longer tented on either side. In the new Solder Mask plots I have corrected the problem of the missing mask clearance on the Bottom side for the vias under: U504, U507 and DCDC9 (and U503). These vias are no longer tented on either side. Debron, as per via plugs, I had included plugs in the obvious locations where I assumed that there would be a problem of solder wicking into vias, e.g. - plugged the thermal/ground vias from the top side in the large center pad of the QFN packages - plugged vias that are very close to an SMD pad where I thought that the line of Solder Mask separation could be too thin to prevent wicking Note that I have generated a new set of Plug plots that now include Plugs from the Top side for the vias under the 10 Ethernet Transformer components. My concern is that these Hub pcb vias are directly under a soldered wire connections on the Ethernet Transformers and I assume that the solder could wick out of the wire connection on these Transformers and into the via in the Hub PCB. Are there any other vias that you would like plugged to facilitate assembly ? e.g. under the BGA components as mentioned above. Issue #7 On outer layers under the back drilled locations we have changed the copper pads to drill + 4 mil so that the pads will be totally removed at final by back drill holes. Please advise whether this is acceptable. Answer: Yes, accepted, this makes good sense. On the back drilled vias, on the side that the back drill is made from, you are adjusting the pad diameter so that the surface pad is completely removed by the back-drill. Issue #8 We are unable to plug the via holes from both sides. As per our process for via holes that are tented by solder mask on one side and opened on the other side, we will do the button print plugging from the tented side with a mask relief of drill + 6 mil. Please advise if this is acceptable or not. Answer: Debron, the whole topic of plugging vias has to do with preventing solder wicking into the vias during assembly. Whatever works for you is fine with me. Can we discuss this during a conference call. I'm happy to modify the design to add or remove plugs on either side. Whatever plugs make for the best assembly is fine with me.